Feed and Speed for slitting Saw ..HELPPPP!!

[Jimic]

I am up against the wall again.BREAKING tools !!

Please give me some "brain" how to mill this part. Before my $SS hit the road. AGAIN !!

 

I have to mill .030 slot, .150" deep. Only 1" lenght but 400 slots per part.

 

Matl: A2

Slitting Saw size: 1/3" thickness. 2.25" Dia HSS

 

What is the Feed and Speed?

How deep per cut to get down to .150" deep ?

 

When the part done. Beer on me this time. All you can drink. :-) Thanks, I know I can count on you. You never let me down before. I wish you are my mother-in-law

[somename75]

hopefully someone with more experience than me will respond, but I would try 50 surface feet, and .0005 per tooth to start. Hope that helps

[Tim Johnson]

I would start at about 100 rpm and conventional cut. If you're using a concave slitting saw (about 36 teeth) .0005 sounds about right. If you're using a screw slotting saw (132 teeth) I would try .0002 per tooth with 3 depth cuts.

[Guest]

+1 Tim

 

very good starting numbers

[Jimic]

My tool is :

High Speed Steel, Screw Slotting Saw

60 teeth

 

Shall I try to run Speed :100 RPM Feed: F1.5

.05" deep per cut ?? Using G41 ??

[jeff]

Does it have to be a slitting saw?

Seems like a woodruff cutter would be alot cheaper.

[David from FN MFG.]

+1 on conventional mill and S & F. that would be really close to where i would start also.

[Storkman]

Free Beer???????

[Tim Johnson]

quote:

---

Shall I try to run Speed :100 RPM Feed: F1.5

.05" deep per cut ?? Using G41 ??

---

Speed/feed & doc sounds ok. I would try G42.

[KEVCAM]

As mentioined above..

 

I would start at about 100 rpm and conventional cut. If you're using a concave slitting saw (about 36 teeth) .0005 sounds about right. If you're using a screw slotting saw (132 teeth) I would try .0002 per tooth with 3 depth cuts.

 

I agree good place to start.

 

Was that Canadian Beer.... right.??

 

Cheers

[Gramby]

You got a problem their 400 slots 1 inch in length and a HSS cutter in A2 steel. Not good at all, hope your only doing 1 part. Otherwise you need a new method. Could this be set up on edge and wired ?

HSS in A2 would be around 50 sfm. chip load .0003 - .0006. 60 teeth you say 2.250 dia. cutter.

Thats 84 RPM at 2.5 ipm with your lead in and lead out length it is going to take you 400 minutes of machining for 1 pass alone. You take 3-4 passes and your talking 1200 -1600 minutes or 20 - 26 hours. No way your cutter going to hold up. 400 slots is your main problem.

[Jack Neelands™]

+1000 Gramby

That HSS cutter wont last you one part

Burn it ...get an edm and make the electrodes and you can rough them and burn them with two electrodes...especially A2...even carbide wont hold up if you have more than one part...you may be looking at 4 hours of machining and setup for electrodes then another 2 hours for setup in the EDM then 4 to 6 hours of burning depending on the the surface finish required

[Jimic]

EdM cost too much. Those slot are for ventalation purpose. Not critical. I have two parts to machine. Now the job is on hold. I might have to get a Carbide Slitting slot.

 

What will be the Feed and Speed if i found a Carbide tool ?

[Jack Neelands™]

where are you located in Ontario jimic ...maybe i can hook you up then ...we cut a stainless alloy with a carbide slitter that last for about a few hundred cuts but not as thin as that ...i can direct you to the right dealer ...jesus that sounded too much like a drug deal

[Jack Neelands™]

The company is called Nova sales hear in London and they supply us with a 2.00 slitter called "SO Carbide" that has a spring lock mandrel

[Gramby]

Uncoated carbide same size , teeth etc should be able to run 3 times as fast as HSS. I would still be concerned for you.

EDM wire or electrod still may be the way to go. No its not cheap. But a .030 x .150 deep slot is not a easy thing 400 times per part. If a designer designed such a costly design they are going to have to pay. Otherwise the deisgner for this company should be looking at machining praticalness. If this is a air slot 3/32 wide .150 would be a piece of cake. Even 1/16 wide .150 deep wouldn't scare me " I'd have to check into cutters". It being A2 I assume it may get heat treated. So I would look at using a 1/16 or 3/32 Carbide ball endmill and use a contour ramp tool path stepping down .005 - .010 increments and going like hell. The ball because of Heat treat cracking issues.

 

Otherwise EDM. Please let us know what becomes of this. GOOD LUCK

[Jimic]

Jack. We are loacted in Cambridege ,Onatrio.Our supplier is SOWA tools. This morning our purchasing agent called them. It sound like they don't have the Carbide saw in house. But, they will find one and give us the quote.

 

Those part are for Toyota plant.Appearancely, nobody wanted the job. It ended on my desk. My boss told me this job have been passed from shops to shops. By the time every shop take a cut and we ended up nothing.

[Jack Neelands™]

yes it looks like you ended up with the short straw on that one...im sorry to hear that